Beam Elements

A beam element is a slender structural
member that offers resistance to forces and bending under applied loads.
A beam element differs from a truss
element in that a beam resists moments (twisting and bending) at the connections.

These three node elements are formulated in three-dimensional space.
The first two nodes (I-node and J-node) are specified by the element geometry.
The third node (K-node) is used to orient each
beam element in 3-D space (see Figure 1). A maximum of three translational
degrees-of-freedom and three rotational degrees-of-freedom are defined
for beam elements (see Figure 2). Three orthogonal forces (one axial and
two shear) and three orthogonal moments (one torsion and two bending)
are calculated at each end of each element. Optionally, the maximum normal
stresses produced by combined axial and bending loads are calculated.
Uniform inertia loads in three directions, fixed-end forces, and intermediate
loads are the basic element based loadings.

Figure 1:
Beam Elements

Figure 2: Beam Element Degrees-of-Freedom

Caution

The mass moment of inertia
about the longitudinal axis, I1
is not calculated for beam elements. Only the m×R2
effect is considered, where R is the distance from the reference point
to the element. The mass moment of inertia about the other axes, I2
and I3,
are calculated based on the slender rod formula (I2
= I3
= M×L2/12).
This would affect any analysis type that includes angular acceleration
loads or effects.

Most
beams have a strong axis of bending and a weak axis of bending. Since
beam members are represented as a line and a line is an object with no
inherent orientation of the cross section, there needs to be a method
of specifying the orientation of the strong or weak axis in three-dimensional
space. This orientation is controlled by the surface number of the line.

More specifically, the surface number of
the line creates a point in space, called the K-node. The two ends of
the beam element (the I- and J-nodes) and the K-node form a plane (see
Figure 3). Beam elements are defined by the local axes 1, 2 and 3, where
axis 1 is from the I-node to the J-node, axis 2 lies in the plane formed
by the I-, J- and K-nodes, and axis 3 is formed by
the right-hand rule. With the element axes set, the cross-sectional properties
A, Sa2, Sa3, J1, I2, I3, Z2 and Z3 can be entered appropriately in the
"Element Definition"
dialog.

Figure
3: Axis 2 Lies in the Plane of the I-, J- and K-nodes

For example, Figure 4 shows part of two models,
each containing a W10x45 I-beam. Note that both members have the same
physical orientation; that is, the webs are parallel. However, the analyst
chose to set the K-node above the beam element in model A and to the side
of the beam element in model B. Even though the cross-sectional properties
are the same, the moment of inertia about axis 2 (I2)
and the moment of inertia about axis 3 (I3)
need to be entered differently.

Table 1 shows where the K-node occurs for
various surface numbers. The first choice location is where the K-node
is created provided the I-, J- and K-nodes form a plane.
If the beam element is colinear with the K-node, then a unique plane cannot
be formed. In this case, the second choice location is used for that element.

The surface number, hence the default orientation, can be changed by
selecting the beam elements using the "Selection:
Select: Lines" command and right clicking in the display area.
Select the "Modify Attributes.."
command and change the value in the "Surface:"
field.

In some situations, a global K-node location
may not be suitable. In this case, select the beam elements in the FEA
Editor environment using the "Selection:
Select: Lines" command and right click in the display area.
Select the "Beam Orientations: New.."
command. Type in the X, Y and Z coordinates of the K-node for these beams.
If you want to select a specific node in the model, click on the vertex,
or enter the vertex ID in the "ID"
field. A blue circle will appear at the specified coordinate. Figure 5
shows an example of a beam orientation where you would wantto define the origin as the k-node.

Figure 5:
Skewed Beam Orientation

The
direction of axis 1 can be reversed in the FEA Editor by selecting the
elements to change ("Selection:
Select: Lines"), right-clicking, and choosing "Beam
Orientations: Invert I and J Nodes". This ability is useful
for loads that depend on the I and J nodes and for controlling the direction
of axis 3. (Recall that axis 3 is formed from the right-hand rule of axes
1 and 2.) If any of the selected elements have a load that depends on
the I/J orientation, the user is prompted whether the loads should be
reversed or not. Since the I and J nodes are being swapped, choosing "Yes"
to reverse the input for the load will maintain the current graphical
display; that is, the I and J nodes are inverted, and the I/J end with
the load is also inverted. Choosing "No" will keep the original
input, so an end release for node I will switch to the opposite end of
the element since the position of the I node is changed.

The orientation of the elements can be displayed
in the FEA Editor environment using the "View:
Options: Element Orientations" command. The orientation can
also be checked in the Results environment using the "Display
Options: Show Orientation Marks: Element Orientations" command.
Choose to show the "Axis 1",
"Axis 2", and/or "Axis 3" using red, green,
and blue arrows, respectively. See Figure 6.

The "Sectional Properties"
table in the "Cross-Section"
tab of the "Element Definition"
dialog is used to define the cross-sectional properties for each layer
in the beam element part. A separate row will appear in the table for
each layer in the part. The sectional property
columns are:

A: Specify the cross-sectional
area in this column. This is the area of the beam resisting the axial
force (d=FxL/(AxE)).
This area must be greater than 0.0.

J1: Specify
the torsional resistance in this column. The torsional resistance is the
area moment of inertia resisting the torsional moment M1. The angle of
twist within an element is calculated by q=M1xL/(J1xG)
where L is the length and G is the shear modulus. For most cross-sections,
the torsional resistance is much less than the polar moment of inertia.
(For a circular section, J1 equals the polar moment of inertia.) The torsional
resistance must be greater than 0.0.

I2: Specify
the area moment of inertia about the local 2 axis in this column. (This
is also referred to as I2-2.)
The local 2 axis passes through the neutral axis of the cross section
and is in the plane formed by the element and the k-node (see paragraph
above). The moment of inertia must be greater than 0.0.

I3: Specify
the area moment of inertia about the local 3 axis in this column. (This
is also referred to as I3-3.)
The local 3 axis passes through the neutral axis of the cross section
and forms the right-hand rule with the element (axis 1) and axis 2. The
moment of inertia must be greater than 0.0.

S2: Specify
the section modulus about the local 2 axis in this column. The section
modulus is calculated from S2=I2/C3max, where C3max is measured parallel
to the 3 axis from the neutral axis to the furthermost point on the cross
section. This value is not required but is necessary for the bending stress
calculation about axis 2 (=M2/S2). If this value is 0.0, the bending stress
about the local 2 axis will be set to 0.

S3: Specify
the section modulus about the local 3 axis in this column. The section
modulus is calculated from S3=I3/C2max, where C2max is measured parallel
to the 2 axis from the neutral axis to the furthermost point on the cross
section. This value is not required but is necessary for the bending stress
calculation about axis 3 (=M3/S3). If this value is 0.0, the bending stress
about the local 3 axis will be set to 0.

Sa2: Specify
the shear area parallel to the local 2 axis. The shear area is the effective
beam cross-sectional area resisting the shear force R2 (shear force parallel
to axis 2). If the shear area is 0.0, the shear deflection in the local
2 direction is ignored (usually a safe assumption). The shear area correction
is only needed if the beam width is comparable to the beam length.

Sa3: Specify
the shear area parallel to the local 3 axis. The shear area is the effective
beam cross-sectional area resisting the shear force R3 (shear force parallel
to axis 3). If the shear area is 0.0, the shear deflection in the local
3 direction is ignored (usually a safe assumption). The shear area correction
is only needed if the beam width is comparable to the beam length.

Note

Hand
calculations for the deflection of beams rarely include the effects due
to shear within a beam. For example, the well-known equations for the
maximum deflection for a cantilever beam and simply supported beam due
to a point load (FL3/(3EI)
and FL3/(48EI),
respectively) only consider the bending effects. If shear effects are
included in the finite element analysis by entering values for Sa2 and
Sa3, the calculated displacements can be higher than the hand calculations.

If you know the dimensions of the cross-section instead of the properties,
you can use the cross-section libraries to determine the necessary values.

In order to use the cross-section libraries, you must first select the
layer for which you want to define the cross-sectional properties. After
the layer is selected, press the "Cross-Section
Libraries..." button.

How to Select a Cross Section from an Existing Library:

Select
the desired library in the "Section
database:" drop-down box. Multiple versions of the AISC Library are provided with the
software. (Note: The AISC library is set so that
the IYY from the AISC manual corresponds to I2 in the software.)

Select
the desired cross section type using the "Section
type" pull down. The types available for each database are
given in Table 2 below.

Select
the desired cross section name in the "Section
name:" section. You can search for a name by typing a string
in the field above the list.

Review
the values in the "Cross-sectional
properties" section. If these are acceptable, press the "OK" button. Note that the
AISC library may not have all of the values needed to perform an analysis.

AISC 2005 &
2001

AISC Rev 9

AISC Rev 8 &
7

Shape

W

W Type

W Type

W shapes

M

M Type

M Type

M shapes

S

S Type

S Type

S shapes

HP

HP Type

HP Type

HP shapes

C

C Type

C Type

Channels - American Standard

MC

M Type (MC)

M Type (MC)

Channels - Miscellaneous

L

L Type

L Type

Angles - equal legs

L

L Type

UL Type

Angles - unequal legs

WT

WT Type

WT Type

Structural tees cut from W shapes

MT

M Type (MT)

M Type (MT)

Structural tees cut from M shapes

ST

S Type (ST)

S Type (ST)

Structural tees cut from S shapes

2L

2L Type

DL Type

Double angles - equal legs*

2L (LLBB on end of name)

2L Type (first dimension is back-to-back
dimension)

UD Type (UDL)

Double angles - unequal legs* (long
legs back to back)

2L (SLBB on end of name)

2L Type (first dimension is back-to-back
dimension)

UD Type

Double angles - unequal legs* (short
legs back to back)

Pipe (schedule on end of name)

P Type

S Type (SP, schedule on end of
name)

Pipe - STD standard weight

Pipe (schedule on end of name)

P Type (PX)

S Type (SP, schedule on end of
name)

Pipe - XS extra strong

Pipe (schedule on end of name)

P Type (PXX)

S Type (SP, schedule on end of
name)

Pipe - XXS double extra strong

HSS

TS Type

RTU

Structural tubing - rectangular

HSS

TS Type

S Type (STU)

Structural tubing - square

Table
2: AISC Library "Section Type"If the section name differs from the type, it is noted in parentheses (
).* When 4 numbers are given, the fourth number is the distance between the
legs of theangle. For example, the 2L8x4x7/8x3/4LLBB are double 8x4 angles, 7/8 inch
thick legswith the long legs back to back and separated by 3/4 inch.

Note

In order to visualize the beam cross section in the
Results environment, the cross section must be chosen from the AISC 2001
or AISC 2005 database.

The AISC 2005 database corresponds to the data in the
Thirteenth Edition of the AISC
Steel Construction Manual.

In addition to the cross-sectional properties, the only other parameter
for beam elements is the stress free reference temperature. This is specified
in "Stress Free Reference Temperature"
field in the "Thermal"
tab of the "Element Definition"
dialog. This value is used as the reference temperature to calculate element-based
loads associated with constraint of thermal growth using the average of
the nodal temperatures. The value you enter in the
"Default nodal temperature" field in the "Analysis
Parameters" dialog determines the global temperatures on nodes
that have no specified temperature.